To
determine your current version, go to Help>About PCB Artist.Version 1.2.2 is required at the minimum to
use the online library.

To
download the latest patch, go to Help>Check For Updates and push the Check
For Updates Now at the bottom of that dialog.

oIt is also good practice to make sure that the
“When To Check” toggle is set to “Once A Day” or “Every time I Start”.

oA web page will launch to the update page.There will be a link to the latest full
installation and the latest Patch.If
your revision is older than both, you must install both.First the full installation, then the patch.

oExit PCB Artist before installing either.

If your
version of PCB Artist does not show the Check For Updates option under the Help
menu, the version pre-dates that patch system.It is best to download the latest complete install from www.pcbartist.com.

Searching
the Online Library:

All
parts in the database are referenced by Part Number and Manufacture primarily.

Digi-Key
part numbers are available for a large percentage of parts, but manufacturer
part number on every part in the library.

Searches
with Attributes can help in filtering, but attributes are not available for all
parts.

For a
comprehensive search by attribute, it is recommended to search on the
manufacturer or distributor’s search engine.This will result in a list of part numbers of suitable parts that can be
used to search the Online Library.

Be
aware that new designers can be deceived by common names that do not indicate
similar packages.For example many
packages are called SOIC-16 and they are usually not compatible with other
SOIC-16 footprints.

Search
Filters can be set to Starts With, Contains and Is Exactly.For the best results, it is often advisable
to use Contains.

The
Reset button clears all fields back to default.

The
Clear Text Button will clear entered text, but not filter and Attribute
settings.

The
Attributes fields require that an attribute is chosen on the left and also that
search text be entered on the right text blank.If not, the search will not proceed.Here is an example of a valid search:

Searches
will display a maximum of 15 parts per page.Links are available at the bottom of the page to continue to other pages
of the search.

Click
on a part in the list to see its available details.

In the
details page, there is a Download and Email To button for retrieving the
part.

oThe Download button will immediately download the
part.It can be saved to any directory
or to your desktop.

oThe Email To button requires that an email address
is entered in the text box to the right.Enter your email button in that box first and then push the Email To
button.When the email arrives, the part
will be an attachment to that email.Save it to any directory or to your desktop.

If The
Part is Not Found:

Makes
sure the search was made from the manufacture’s part number from the Part
Number search field with the filter set to Contains.

There
are over a quarter million parts in the online library, but there are tens of
millions of parts/packages in circulation.

It
takes less than 5 minutes to make most parts in PCB Artist.It is not efficient to spend much more time
than that searching for parts; the part could have been made already.

For a
tutorial in making a part, go to Help>Tutorials>Part Creation Tutorial in
the PCB Artist main menu.

oTypically, a part such as a microcontroller is very
easy to create because the wizards can be used to make all three parts.The PCB Symbol for a microcontroller can be
created in the wizard in about 30 seconds once you have experienced creating 2
or 3 of them.

The
Frequently Asked Questions document also has a topic link in that sectionthat details how to manually create parts
that cannot be created in the wizard (such as switches and connectors, which
have no common form factor for the wizards).Manual part creation is covered in the “How Do I Create A Connector Or
Other Manually Created Parts” topic link, just under the walkthroughs of the
three symbol wizards.

Importing
the Part to PCB Artist:

From
this point the part has been downloaded from the Online Library to a directory
or to your desktop.

The
file will have the .palib extension.That file is a medium for transporting, in one package, the schematic symbol(s),
PCB symbol(s) and the component itself that defines the relationship and pins
of the symbols.

To
bring the part into PCB Artist, simply select the .palib file and drag it into
PCB Artist.

When
the file is dropped onto PCB Artist, the application will take from that file
the symbols for the part and put them into the schematic, PCB symbol and
component libraries.

The
contents of the .palib file will be imported to the following directories:

oThe schematic symbol(s) will go to the library
$Download.ssl.

oThe PCB symbol(s) will go to the library
$Download.psl.

oThe Component will go to the library $Download.cml.

oThis is the import dialog:

If the
part is to be immediately used, the application may not immediately recognize
the new symbols in the library.To have
the application rescan the libraries to find the new parts, change the current
working library to [All Libraries].This
will cause the application to scan and re-index all libraries and find the new
parts.This only needs to done once in
any of these three locations:

oFrom the Library Manager, change this drop down
menu to [All Libraries]:

oFrom the Interaction Bar (which is brought up with
F9), change this drop down menu to [All Libraries]:

oFrom the Add Component dialog, change this drop
down menu to [All Libraries]:

oFrom any of the three dialogs, change your library
to $Downloaded.psl to use the newly downloaded part.

oOnce the part is imported, the .palib file can be
discarded or filed in a folder.

Verify
the Part:

It is
recommended to verify all parts before use, regardless of the source the part
came from.

Finding
the Names of the Symbols in the Component.

oBring up the Library Manager, click on the
Component Tab at the top of that dialog and change the Library drop down menu
at the top of the dialog to $Downloaded.psl.

oIn the left of the dialog there will be a list of
the components in that library.Select
the part you downloaded.

oIn the right-hand side of the dialog, the name of
the symbols the component uses are listed.Note those symbol names for later reference, they must also be
verified.

Verifying
the Component.

oBring up the Library Manager, click on the
Component Tab at the top of that dialog and change the library to
$Downloaded.psl.

oIn the left of the dialog there will be a list of
the components in that library.Select
the part you downloaded.

oClick the Edit button in the central column of
buttons.

oThis is the Component Editor.In this screen you can verify the pins
mapping, the logic names and any implied nets assigned to pins.Multiple gate pin mapping is also done on
this screen.

·The Gate Name is used to identify individual
schematic symbols on parts that have multiple schematic symbols (referred to as
gates).Most symbols will not have
multiple gates.

·The Sch Symbol Name column identifies the schematic
symbol for that gate.

·The Sch Symbol Terminal Name column is where logic
names can be entered for the part.If
none are assigned, they can be entered here and saved with the part.

·The Sch Terminal Number, PCB Symbol Pad Number and
the Component Pin Name/Number columns map the relationships of the pins between
the symbols.This should be confirmed.

·The Net (Class) Name can provide an automatic
implied net for a particular pin.In
this column a pin can be added to the GND net, for example.Be aware there are sometimes implications
with specific implied nets that can affect future designs.For example, if a net is assigned to GND, and
is later added to a design where the ground net is named AGND.In that case the GND net will be a new net
and not connected to AGND.

§For more information on the Net (Class) column and
it options for creating implied nets and also implied net classes, go to
Help>Contents in the application.In
the upper left, click on the Index tab and search for the term Library
Components.

Verifying
the Schematic Symbol.

oClick on the Schematic Symbols tab in the upper
left of the Library Manager.

oChange the Library drop-down at the top of the
dialog to $Downloads.

oClick on the symbol for the part you downloaded
(determining that symbol name is described above in Finding The Names Of The
Symbols In The Component bullet at the top of this section).

oThe part will preview on the right if the Preview
checkbox is clicked on.

oTo edit the part, click the Edit button.

oGo to File>Save to keep any changes made.

Verifying
the PCB Symbol.

oClick on the PCB Symbols tab in the upper left of
the Library Manager.

oChange the Library drop-down at the top of the
dialog to $Downloads.

oClick on the symbol for the part you downloaded
(determining that symbol name is described above in Finding The Names Of The
Symbols In The Component bullet at the top of this section).

oThe part will preview on the right if the Preview
checkbox is clicked on.

oTo measure features or edit the part, click the
Edit button.

§The Measure tool is located under Tools in the main
menu.

§For through-hole parts, the pad Width dimension
must be .014” over the hole size to pass annular ring checks.This is best determined from Settings>Styles
in the Pads tab.

§Verify all dimension of the part.

§The footprint can be printed from File>Print,
set the scale to 100.It is a good
practice to put a sample on the print out to verify the footprint.

oDimensions and diagrams on the part will not appear
on the PCB and do not have to be deleted from the part.